MS05000 Budget Logic Analyzer Probe Set Design

[Gandalf_Sr]

Design Aim
The design aim is for a budget LA probe for the MSO5000 that can be built to work in 2 positive voltage ranges:

1. 0.65V - 3.6V logic levels using a SN74AXC8T245 as U3 on the probe PCB - probably at 100 MHz or more (to be tested) but tested at 50 MHz.
2. 1.6V - 5.5V logic levels using a SN74LVC8T245 as U3 on the probe PCB (and other minor component differences) - tested at 50 MHz.

The official Rigol connector (PLA2216) uses expensive Op Amp ICs that can (theoretically) work up to 15V and 1GHz but they cost $400 a set ($350 if bought with the scope) and the scope LA input is only specified up to 200 MHz.

Project Status
The design is finished, the 3.3V version of the probe PCB has been built and tested at 50 MHz. I have ordered a load of PCBs so if you want a set, look at this post and PM me with what you need.  Then go and check out this post that has links to Digikey carts that will allow you to buy all the parts needed. The schematics in .pdf an BOM in Excel are here.

High Level Summary
The design uses 2 different PCBs:
1. A passive (no active components) Connector PCB that adapts from the MSO's 50-pin 0.1" header (J1) to 2 x 0.1" pitch 24-pin headers that take standard ribbon cables.
2. Two Probe Adapter PCBs that convert the sensed logic signals into LVDS which they drive into the ribbon cables.

Each probe PCB has an 8 bit voltage level translator (VLT) IC followed by 2 x 4 bit LVDS driver ICs.  The LVDS driver ICs and the output (B) side of the VLT run at 3.3V which is supplied by a 3.3V, 300 mA LDO regulator (that supply is also available for your use on the 3.3V test pin).  The input (A) side of the VLT is powered from an adjustable 0.6V to 3.9V, 100 mA LDO regulator (that supply is also available for your use on the Vadj test pin).


Probe Adapter PCB
This description is for the 0.65-3.6V version (with the 1.6-5.5V version differences shown in parentheses); the 3.3V LVDS signals these boards output are the same and any combination of probe PCBs can be attached to the Connector PCB.
Eight logic sensing leads connect to J1 feed into the A side of a SN74AXC8T245 (SN74LVC8T245) which is an 8-bit voltage level translator (VLT) that can range from 0.65 to 3.6V (1.6 to 5.5V) operating voltage. The VLT is hard-wired to make the A side the input and the B side th eoutput.  The outputs on the B side of the VLT run at 3.3V and feed a pair of DS90LV047A LDVS driver ICs that drive the LVDS signals to the Connector PCB via the 24-pin header connectors and ribbon cable.

There are 2 separate power supplies on the Probe PCB both fed by the 4V line passed from the Connector PCB:
1. A 300 mA 3.3V fixed LDO linear regulator that supplies the DS90LV047A LDVS drivers and VccB on the SN74AXC8T245 (SN74LVC8T245).
2. A 100 mA LDO that is adjustable from 0.65 to 3.6V which supplies Vadj.

A switch selects what voltage is fed to the VccA side of the VLT IC, U3; it selects between Vadj or Vext (an external voltage that you have to feed in on a pin on J1).  This allows the device under test (DUT) to be powered by Vadj up to 100 mA (the level translator IC uses uAs) or for the DUT to provide the power to VccA. The max voltage that should be fed into the Vext pin is 3.6V (5.5V) but a protection Zener diode protects the SN74xxx8T245 VccA side.  To monitor logic at voltages greater than 3.6V on the SN74LVC8T245, VccA must be sourced from the Vext pin because the Vadj supply only goes up to 3.6V (YMMV but the limit is the actual 4V level from the scope and the drop over the LDO regulator).  Note that the level adjustments available on the MSO5000 menus don't do anything as the input resolution of a 1 or 0 is related to the VccA applied to U3.

The Probe PCBs are only 2 layer; I ran impedance calculations for the 2-layer PCB and it comes out around 130 for 1.6mm FR4 and my trace widths so I think it will be OK up to 100 MHz or so.

200 series resistors (R0-R7) provide basic protection to the inputs to the SN74AXC8T245 and there are also optional 10k load resistors (R13 - R20) on each input. Care should be taken not to overvolt the inputs or U3 could be damaged.

The Connector PCB
This is 4-layer passive circuit that routes the LVDS signals coming from the Probe PCBs to the front connector on the MSO5000. The pairs of LVDS signals are length matched to <3mm and the channels are all within 10 mm of each other. The traces have been moved to be on the same side for each LVDS pair (as far as possible) and have curved traces to avoid reflections (all probably overkill for 100 MHz).

The latest schematics are attached to this post.

[Edit1] Upload of .pdfs schematics
[Edit2] 2/28/20 to reflect 5V option and protection components
[EDIT3] 3/8/2020 major update of all text to reflect design changes and build status
[EDIT4] 3/14/2020 first & second posts updated to show working status and pictures of it running
[EDIT5] 3/21/2020 updated to reflect the choices made for input protection on Probe/Connector vn1b2/1a4 PCBs
[EDIT6] 3/23/2020 updated to delete the schematics attached to this post and point to the latest ones
[EDIT7] 3/28/2020 added more detail to the circuit description
[EDIT7] 4/28/20 added link to post that has zipped schematics and BOM
[EDIT8] 5/2/20 changed VccIO to Vext to match markings on Probe PCB
[EDIT9] 5/21/20 minor changes to enhance readability and clarity

[thmjpr]

maximum logic level voltage of 3.6V (4.2 absolute max)

]

If you are saying it will be damaged when going above 4.2V, I would consider adding some resistor protection. At least to prevent the thing from being blown up, if you inadvertently touch the probe to a 5V rail say.

I would say enjoy the cruise, but yeah this is probably more interesting for you

[Gandalf_Sr]

[EDIT] Here are the pictures of the finished 3.3V version running at 10 MHz.

[Gandalf_Sr]

maximum logic level voltage of 3.6V (4.2 absolute max)

]

If you are saying it will be damaged when going above 4.2V, I would consider adding some resistor protection. At least to prevent the thing from being blown up, if you inadvertently touch the probe to a 5V rail say.

I would say enjoy the cruise, but yeah this is probably more interesting for you

It's ages since I looked at any 5V logic.  The issue I have run into recently is being able to handle sub 3.3V logic levels, this setup goes all the way down to Vcc at 0.65V.  Adding a simple voltage divider to deal with 5V logic should be very simple.

[EDIT} Keep reading as the design was enhanced to allow use of a LVC VLT IC to handle up to 5.5V logic levels.

[texaspyro]

It's ages since I looked at any 5V logic.

Supporting 5V levels wou;d be a very good thing (I'd consider essential for any logic analyzer).  There is a LOT of older 5V equipment (and Arduinos) out there that need an occasional probing.

[Gandalf_Sr]

I hear you 5-volters and have just looked at using the LV4T family (e.g. SN74LV4T125) which would allow me to range between 1.2V and 5V on the input voltage side, I've asked for advice on TI's e2e forum but the LV4T devices will use a bit more power and only work at 50 MHz max.

[EDIT] If U3 on the Probe PCB is changed to a SN74LVC8T245 and R10 made 0 then the PCB (with no modifications) can run between 1.6V and 3.9V using the onboard Vadj LDO supply or you can feed an external 5V in to run the logic at 5V levels. With this change you lose the ability to go as low as 0.65V logic levels and you will have to supply an external VccA because you can only supply VccA with up to 3.9V Vadj from the Probe PCB, and you can only go up to 50MHz (has been tested OK at 50 MHz) - That was easy

Unless TI suggest something else, we can build 0.65 - 3.6V and 1.6V - 5.5V versions of the Probe PCB on the same bare board; you can mix a 0.65V - 3.6V probe (8 channels) and a 1.6V - 5.5V probe (another 8 channels) plugged into the Connector PCB at the same time.

Note that the Vref signal from the MSO5000 is not used.  The only power supply that's used from the MSO5000 is the +4V which is fed through a 1210 component (mounted on the Connector PCB) that can be a resettable fuse or a ferrite bead inductor (or a 0 resistor); it seems to me that the MSO5000 will almost certainly have some sort of current protection on the +4V supply so my inclination is towards a ferrite bead inductor.

[Gandalf_Sr]

Update...

I have tweaked the PCB designs for the cheap LA probe hardware, the connector PCB now has all LVDS pairs routed on the same side (as much as possible) and the traces are all curves.  The probe PCB has minor improvements and both PCBs have loads of ground vias added to stitch around the edges of the LVDS signals.

I am waiting for a parts delivery from Digikey so I can check some footprints before ordering the PCBs. The passive, 4-layer (LVDS) Connector PCB adapts the MSO5000 down to two 24-pin 0.1" headers each carrying 8 channels of LVDS data.  There are 2 identical, 2-layer probe PCBs which use 8 channel voltage level translators (can be one of 2 types) feeding into 2 x LVDS driver ICs (4 bits each) per Probe PCB that drive the LVDS signals into more 24-pin 0.1" headers that feed the ribbon cables and on to the Adapter PCB which, as far as the signal path is conerned, has nothing but LVDS terminating resistors.

Each probe PCB can be fitted with one of two different voltage level translators; one allows a VccIO range of 0.65 - 3.6V and the other allows 1.6 - 5.5V; you can have one of each if you want to.

Total BOM cost for the whole setup (2 x probe and 1 x connector PCB) is about $25 in components plus the cost of the PCBs - maybe another $20.  I deliberately kept everything at 0603 and 0.65 mm pitch TSSOP (ICs with legs) so that it can be hand-assembled by those comfortable with SMT assembly.

[texaspyro]

If you have room for 0805's it makes it considerably eassier to hand assemble...

[Gandalf_Sr]

If you have room for 0805's it makes it considerably eassier to hand assemble...

0603 is my standard size for hand assembly although I do work under a stereo microscope.  I should have added that I'm trying as much as possible to maintain signal integrity and IMHO 0603 is better than 0805 in this respect (0402 would have been better still but they are more difficult to work with).

My MSO5074 arrived a week ago but has been RMAed as they sent me old stock (Cal date 3/18/2019), a new (hopefully) one will arrive tomorrow.  JLCPCB are back at full production so, once my Digikey order arrives, I can check the footprints and order the PCBs; then it will be a couple of weeks before they arrive.

[texaspyro]

I should have added that I'm trying as much as possible to maintain signal integrity and IMHO 0603 is better than 0805 in this respect (0402 would have been better still but they are more difficult to work with).

At the frequencies involved in the probe (200 MHz) the 0805 package size is totally acceptable. 

[Gandalf_Sr]

I should have added that I'm trying as much as possible to maintain signal integrity and IMHO 0603 is better than 0805 in this respect (0402 would have been better still but they are more difficult to work with).

At the frequencies involved in the probe (200 MHz) the 0805 package size is totally acceptable.

I know it's overkill but I was trying to observe the LVDS routing rules with 0.3 mm trace width/gap and then not have a massive flare when it arrives at the terminating resistor just before going to the scope connector.

Quit your nit-picking or I'll make them 01005s 

[Gandalf_Sr]

I got the Digikey order and checked some footprints, I'm glad I did as I didn't allow enough width on the headers that are side by side on the connector PCB, this is now fixed along with a few minor changes.  MY MSO5074 arrived today too and I checked the front entry space for the connector PCB, it's OK.

The PCBs were ordered today from JLCPCB, I ordered 5 connector PCBs and 10 probe PCBs; remember that a set is 1 connector and 2 probe PCBs.

Now I have to wait. I'll update the PCB views in a day or so.

[EDIT] The PCBs shipped yesterday and their system predicts they will arrive Friday 13th (my lucky day).  Sorry, still not updated any of the files.

[Gandalf_Sr]

By way of a bump and an update, DHL says that my JLC PCBs departed from Cincinnati (250 miles South of me) at 6:30 am today and they are supposed to get to me by the end of today although that sounds a bit optimistic although possible; the main freight truck will probably get to Michigan around 11 am (unless they are flying them up) and then they'd have to make it onto the actual delivery truck and to my house.  If they don't make it today, they could be delivered tomorrow.
[EDIT] seems the package got to Romulus Michigan in 2.5 hours so, unless they drove it up in a Ferrari at 100 mph, it must've flown up . Yup, it got here around noon and the PCBs look great.

I revisited the documentation on LVDS vs LVPECL and I think that LVDS running at 3.3V and driving into a 100 resistor close to the MSO5000 connector is going to drive the MSO5000 internal circuits OK, I will run a test before I fully populate the PCBs as it may need a 120 resistor - I really hope this is going to work as it could be a show-stopper; I should have tested first but I didn't. Sigh!
[EDIT] I asked over at the other real LA teardown thread and dug into the driver datasheets; the real LA probe set uses LMH7322s which are hooked up, with 2.5V for Vcco, which makes them run with LVDS-compatible outputs with H = Vcco - 1.0V and L = Vcco - 1.4V (centered on 1.2V) which is LVDS-compatible. My design uses DS90LV047As which have LVDS outputs which should be fully compatible with the MSO5000 inputs - we'll see.

I was planning a fun trip to Chicago with my Brother next week but we cancelled due to the COVID-19, weld-yourselves-into-your-houses, panic.  So now I'll be able to work on this unless I get some paid work to do.

[Gandalf_Sr]

IT's ALIVE!!!!! BWAHAHAHAHAHAHAAAA

Go back and see the second post for updated pictures of it running (at 10 MHz).  I only built the 0.65-3.3V probe board so far and the input protection Zeners were missing from my Digikey order so it's running without them for now.

I'm VERY happy with the results so far.  First 8 channels are all the correct polarity and the LVDS signals are clearly working at least at 10 MHz, I tested channels 0-7 so far.

[Sighound36]

Would just like to say this thread is what really good about this forum sharing knowledge and experiences top stuff  Gandolf_Sr.

I just do not have the time to do these sorts of projects at the moment and its great to see 

Promise I will do an update on the 8000 thread soon.

[joeyjoejoe]

Very cool, nice work! 

[Gandalf_Sr]

Total cost for components for 2 probe boards and 1 connector board (including 2 x 6" ribbon cables) is $35.28, if I order say 50 of the PCBs my guess is $1 each for the probe boards and $2 each for the connector boards.

Still doing more testing but here's another picture of the 2 different probe PCBs, the one on the left with the red LED is the 1.6-5.5V version and the one on the right with the green LED is the 0.6-3.6V version.  I triggered it from D4 with a serial signal while feeding a 50 kHz square wave into the other probe board on D11 and D14, the yellow trace is analog Ch1 showing the 50 kHz signal.

[Gandalf_Sr]

Here's an picture of the connector PCB (before I added all the termination resistors).

[EDIT] Did some high frequency tests on the 0.65-3.6V probe PCB running at 3.3V with a 50 MHz square wave from my DG4202; it looked OK but there was an occasional 1 nS jitter on all channels.

I wonder if that was the signal generator?

[Gribo]

What part did you use for the 50 position 0.1" header?

[Gandalf_Sr]

What part did you use for the 50 position 0.1" header?

This one https://www.digikey.com/product-detail/en/sullins-connector-solutions/SFH11-PBPC-D25-ST-BK/S9201-ND/1990094

[Gandalf_Sr]

While the vn 1a boards seem to work just fine, I have a tweak in progress to fix very minor issues, like the adjustable voltage control pot works backwards.  I have a few other tweaks to consider too.

If I order new vn 1b PCBs I can add to the order if anyone's interested? PM me if you want a set.  I'll update the schematics and add the BOM later this week.

[thmjpr]

Here's an picture of the connector PCB (before I added all the termination resistors).

[EDIT] Did some high frequency tests on the 0.65-3.6V probe PCB running at 3.3V with a 50 MHz square wave from my DG4202; it looked OK but there was an occasional 1 nS jitter on all channels.

I wonder if that was the signal generator?

Nice work.
You can see in the specs the LA sample rate is 1Gs/s, so 1ns jitter may be expected.

[Gandalf_Sr]

Here's an picture of the connector PCB (before I added all the termination resistors).

[EDIT] Did some high frequency tests on the 0.65-3.6V probe PCB running at 3.3V with a 50 MHz square wave from my DG4202; it looked OK but there was an occasional 1 nS jitter on all channels.

I wonder if that was the signal generator?

Nice work.
You can see in the specs the LA sample rate is 1Gs/s, so 1ns jitter may be expected.

Thanks, so that suggests that the jitter is not a problem of my design    In reality, there are not many serial data systems that I've designed that run at more than a few MHz so this is likely a non-issue.  My aim was to make it cheap and functional and I think I achieved that.

One thing I haven't found yet is where in the menus I can align the analog and digital signals in time - I thought that was somewhere in the menus?

[NoisyBoy]

Nice, love reading all the great progresses you are making.

[Gandalf_Sr]

Question on Front End Protection
So the probe design is working fine at 50 MHz but I had originally designed in some protection on the front end (see picture).

J1 is the probe input connector and R0-R7 are 200 series resistors and the results I've posted so far are just with those series resistors fitted.

The 3.6V dual Zeners (D2-D5) arrived yesterday and I fitted them but they clearly affect a 10 MHz 3V square wave so they are not going to work and I took them off.

I tried adding terminator resistors R13-R20 but they don't seem to have any affect at all and a TI engineer on the e2e forum thought I didn't need them.  However, the datasheet for the SN74AXC8T245 warns that it shouldn't have floating inputs but the chip seems just fine with just the series resistors and, with nothing connected, the detected level registers as a zero.

I have various FET scope probes that have warnings about maximum voltage.  The schematic shown is for the 3.3V probe version (the 5V version uses an SN74LVC8T245 as U3) and the absolute max input voltage for the SN74AXC8T245 is 4.2V according to the DS so a 5V logic input could fry it (with the LVC version it's 6.5V but the minimum Vcca voltage is limited to 1.65V).  I don't work with 5V logic but I did build a probe PCB that has the 74LVC part in case I ever needed to.

Before I tweak and make V1b of the probe PCBs, what do you guys think I should have at the front end?

1. Just the series resistors and provision for the termination resistors on the PCB so people can populate if they want - you fry it, you change U3.
2. Option 1 but with series and termination resistors fitted - might offer some protection but changes input impedance to 10k
3. Something else???